[anti-random]

Hi, for my bachelor thesis project I have to measure the aerodynamics of a 3d wing in the ground effect. I am able to get my coefficient of lift value to well within 5% of the experimental values however the coefficient of drag always hovers around 10 to 20%. I am wondering on how to improve this.

The model is a NACA 6409 rectangular wing. The chord is 1m and the span is to 2m. The height the airfoil above the ground varies between 0 to 1m. I am using the Omega Reynolds Turbulence model and with a 5% turbulence intensity at the inlet.

So, if someone could recommend ideas of how to improve the drag results it would be greatly appreciated.

[ghorrocks]

Accurate lift but less accurate drag is typical for airfoil simulations. Drag is much harder to get right.

General comments are here: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

But if you are within 5% on lift and 20% for drag then you already have most of the basic stuff sorted. What Re number is the flow at? Why did you choose omega Reynolds turb model? Does your inlet boundary turbulence match the experiment? What about surface roughness?

[anti-random]

Hi Ghorrocks,

The Reynolds number is 300 000. The omega reynolds stress turb model was chosen because a previous cfd study showed that it was the best turb model for a wing in ground effect. Yes, the inlet does match the wind tunnel experiment. The surface roughness was a smooth wall. The ground is a fixed wall because that what was used in the experiment.

I thought it was a mesh issue but I have refined the mesh at the wing quite significantly. The other thing i should mention is that I am using the hybrid mesh in ANSYS. All the outer faces of fluid domain and the wing where meshed using the mapped face feature so they are all quad elements. Should I change the way I have meshed the model?

[ghorrocks]

I have refined the mesh at the wing quite significantly.

Yes, but have you actually done a mesh refinement sensitivity analysis to determine if you are fine enough yet? Read the link for further details.

At Re=300k I would expect the front bit of the wing to be laminar with a transition. To capture this you will need the SST turbulence model with a transition turbulence model. You cannot do this with omega RSM. But whether this is significant or not is up to you to determine - but it will affect the drag.

[anti-random]

I used the SST turbulence model and was able to get a better drag coefficient. I only did this for one simulation and was able to improve my original result. The value was drag value was within 10%.

Now, when I tried to change a parameter in the geometry, ANSYS is unable to even begin solution. It gives me the error:

Partitioning of domain: Default Domain

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| SYMASS_ZONE_EL_PART : The solver ran out of temporary space while |
| building a linked list for a domain. Try setting the expert par- |
| ameter "topology estimate factor" to a value greater than 1.0. V- |
| alues higher than 1.2 should not be necessary. |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine SYMASS_ERROR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX partitioner exited with return code 1.

I am thinking it is related to a meshing error. But the thing is it ran previously. Also, I forgot to mention the parameter in question is the height the wing is from the ground. In the first run it was 20mm and in the current run it is 40mm.

[ghorrocks]

Did you set the parameter recommended in the message?

[anti-random]

I was reading through the documentation which said that for the vast majority of simulations the expert parameters need not be changed. Considering that this is a basic 3d wing simulation I think it is best not to change this parameter yet. I was hoping to fix this problem in another way.

[ghorrocks]

The error probably is related to mesh quality but I cannot be sure. I would just try the parameter it suggests and see how you go. But still worth your while to improve mesh quality.

[anti-random]

Hi, so the problem relates to how CFX estimates the amount of memory it needs to compute the problem. By increasing that value it increase the memory estimation. So, I just cheated and decreased the element number in my model. By this why I can at least try and get a simulation working which I can than refine. Thanks for all the help.